Designing a product is only part of the process. Now, can that product be manufactured? A CNC machinist works with computer numeric controlled (CNC) machines from generating the machine code to machine setup and run. Understanding both CAD and CAM is essential to this portion of a design. Even if you are not the end user who programs a machine, it is invaluable to know how it’s done. This knowledge translates directly to part design by helping make intelligent design decisions with manufacturing in mind. This course introduces you to the integrated CAD/CAM approach behind Fusion 360 CAD/CAM as well as 3D printed design setup and finally assembly and testing. All stages of product design in one place!
After completing this course, you will be able to:
• Explain the Fusion 360 integrated CAD/CAM manufacturing workflow.
• Summarize the trends that are influencing the future of manufacturing.
• Demonstrate knowledge and skills in foundational concepts of Fusion 360 CAD/CAM software.
• Set up a Flight Controller.
• Assemble a quadcopter.
• Fly the final design.

教學方

Autodesk

腳本

In this lesson, we'll be creating both drill and tap toolpaths. After completing this lesson, you'll be able to create a 2D contour toolpath, create a peck drilling operation, and define a rigid tapping toolpath. Let's carry on with the file from our previous example. And let's take a look at a few more 2D operations. We want to select 2D contour. And we want to create a 2D contour that can cut this geometry right here. We're going to carry on using the 10 millimeter flat and mill. And on the geometry section, we want to grab each of these edges. We're going to leave all the rest of the default operations and we're going to take a look at the preview. So you can see here we have the tool coming in, it's leading in, cutting this section, and it's wrapping it up and over, and cutting both on the other side. Now there's a much cleaner way that we can do this, but fusion thinks that this hole is already here, so the edge selection is not allowing us to simply take the tool straight across. If we expand the CAM component, expand the sketches folder, and show sketch eight, we have some lines that were used to create this geometry. So lets edit the tool path. Go back to the geometry, clear the chains, and select the two chains on screen. When we have a situation like this, where we have a single line, it can be a little bit difficult to tell. But we need to make sure that the arrow for the contour is going the direction, and is on the outside of our selection. When it's like this edge, we need to do the same to make sure that we're cutting in the right direction, and we can say okay. So now the preview on the screen has the tool coming in, cutting this section, wrapping it over and coming down. If we really wanted to, we could also create a new sketch that allowed us to keep the tool down the entire time, and wrap around the outside of this contour. But for our purposes, this is not going to take too much extra time for us to do that wrapping movement because it's only one single cut. If you have a lot of these regions to do it, it makes sense to try to keep the tool down as much as possible and keep the feed rate high. Lets click in the canvas area to deselect the tool. Let's take a look at drilling this hole. We're going to select drilling. We're going to change the tool type by filtering the operation, we're going to set it to hole. We're going to change the type of tool, we're only going to use drill and center drill. And we want to turn off our filter for the dimension. We're going to again use the samples library. And we're going to minimize inch, but we're going to look at samples, and we're going to look at aluminum. Now if you want to in the samples library, we can also turn off all of the inch libraries and we can only focus on metric aluminum, and this will give us access to those drill bits. That specific hole is going to be five millimeters, and we're going to have a five millimeter drill. And we can also use a spot drill to start the hole if we need to. Now if we scroll all the way down, we'll get access to the spot drills. But for us, we're going to just go ahead and drill it at five millimeters. The geometry is going to be this hole. You notice that we also have the option to select all holes that are the same diameter. We have our heights. And specifically when we're dealing with holes, we have an offset at the bottom, we also have a drill tip through bottom, we can give it an extra amount of clearance. Now the important thing that we want to focus on here is the cycle. We have a cycle option for doing break through, deep drilling, counterboring, chip breaking, there are very many options inside of here that we can use depending on the type of hole that we're cutting. In this case, we want to use chip breaking. And we want to give it some values for how much to peck any time that we want to dwell before retract, and the amount of time that we want to dwell. So we're going to use a pecking depth of 1.25, we're going to say okay. Now this specific operation is going to come down and it's going to peck a small amount. Now you notice the preview on the screen also shows the size of the hole that's getting drilled in relation to the geometry. Now the reason this is actually showing a larger hole is because this is setup to be tapped, a tap for a five millimeter. So we're going to edit the operation. We're going to change the tool, and we're going to change it to a four and a half millimeter drill bit. So we want to scroll down till we find four and a half, we're going to say okay, and we're going to regenerate that tool path. The next thing that we want to do, is we want to right-click, and we're going to copy this operation, and we're going to paste it. We also have the option to duplicate the operation. But if we right-click on setup one, we can paste it. And notice that we have a second instance of chip breaking. I'm going to edit. And I want to start by editing the tool. In the samples library, the operation is going to be hole, the type. In this case, it's going to be a right hand tap. And what we're looking for is right-hand taps that are for five millimeter. So notice we only have metric aluminum. And if you look at the cutting diameter, you can see the size that we have here, these are number tens. And we get down to the metric section, you see that we have an M5, we can say okay. Under cycle, notice that we have several different types of tapping. We have a simple tapping, left and right, tapping with chip breaking, and if we scroll all the way down we also have thread milling. We're going to use a tapping operation, and we also have a dwell period. So now we've pre-drilled the hole and we're going to be doing a rigid tapping operation on the hole. So at this point, let's go ahead and save our file so we can move onto the next step.